hello all
i'm a machinist for 18 years and just getting into this CNC thing.
the company just brought a benchtop CNC. i've been plating with to learn,
but can't figure out how to setup to tap a 2-56 thd.
i know g84(i'm writing g-codes, can even get the endmill to go where i
want :), but tapping is another whole new universe. any help would be
appreciate, thanks

Hi kenneth, 2-56 is a tiny little tap this may be a challenge in any case.
First make sure you have a floating Tap holder.
This kind of holder will allow the Tap to move a little up or down along the Z-axes to make up for the overrun that will happen when the tap reverses direction at the bottom position.
Next make sure the holes drilled previously are sufficiently deeper then the tapping depth, and located precisely. (may have to centerdrill, drill, champfer first.)
To program the tap cycle I use the following methode.
56 threads per inch could be run as 56 RPM Spindlespeed with 1." Feedrate in Z.
Or as this is very slow you could just multiply both values by a factor example.
4x = 4 x 56 RPM = 224 RPM Spindlespeed and 4 x 1." Feedr. = 4." Feedrate
may be a good place to start.
Be conservative on the Depth this small tap can load up with chips and get stuck and break if you try to go too deep with.
Position R a larger distance above the Part to allow room for the Startup vibrations to subside before the tap enters the material.
To Tap this at X1. Y1. and X2. Y1. with the Top of Material at Z0. and a hole of proper size at least .4 deep, you could program this like this.

S224 M3
G84 X1. Y1. Z-.25 R.4 F4.
X2. Y1.
G80

You may add as many positions between G84 and G80 as you like.
Run this with Speed and Feed override set at 100% only.
I would try this on some scrap pices of the same material first.
The key for those little Taps is to determine how many holes can you Tap before the Tap gets dull and breaks. Then you just change the Tap with a new one before you reach that number.
Good Luck

thank you Torsten,
i have to tap 104 2-56 x .25 deep thd. in 30 parts each.(i'll be busy:)
thanks for your reply.

S224 M3 <----------speed and direction
G84 X1. Y1. Z-.25 R.4 F4.<--x and y your movement..what is r.4 ??????????? f4 = feed
X2. Y1. <---your movement
G80 <---------end tap cycle

how do i calulate r ?


again thanks for your help

thank you Torsten,
i have to tap 104 2-56 x .25 deep thd. in 30 parts each.(i'll be busy:)
thanks for your reply.

S224 M3 <----------speed and direction
G84 X1. Y1. Z-.25 R.4 F4.<--x and y your movement..what is r.4 ??????????? f4 = feed
X2. Y1. <---your movement
G80 <---------end tap cycle

how do i calulate r ?


again thanks for your help

Sorry for getting back so late, I was off for a while.
R is the z-axis coordinate where the Tool will start to feed down from.
in this example Z0. is assumed the Top of the Part so the Tool will start .4" above with the downfeed.